Is the latest Eagle any better at differential routing?

[rx8pilot]

I have been using Eagle for a few years - my latest version is 6.5. In general - I hate Eagle in nearly every way I can hate a piece of software but I cannot afford the time or the money to switch at the moment. I have a well setup library and a growing list of ULP's that tie my manufacturing systems together. Setting that up again is worse than dealing with Eagle for design (at least for now).

One of my biggest challenges is designing high-speed PCB's with various types of transmission lines where the geometry has to be very specific. Differential pairs are a total nightmare to route accurately. This is especially true when you need to make small changes after you manually get a pair routed.

I don't like the new subscription-only model, but will gladly push that aside if I can more easily route high-speed boards. Does anyone have any experience with this type of design using the latest version of Eagle. I have not yet found any videos or articles covering this topic.

[KE5FX]

The MEANDER function in version 7 seems to work well enough once you grok it.  I assume it was the same in V6. 

The autorouter doesn't support differential pairs even in the current Autodesk release, so there's no incentive to upgrade in that regard.

[MarkL]

I'm not sure how sophisticated your differential routing requirements are, but I've been using differential routing (with automatic meander) in 7.2 with no issues.  However, my needs are fairly simple with 10/100 ethernet and HS USB.

According to the release notes, those features were introduced in 6.0.0.

In case you were unaware of the feature:

The basic procedure is to set up the signal names so the pair ends in _P and _N, create a class that defines the trace spacing and the width, and then add the signals to that class.  When you click on one of the signals to route it, it will route both of them at the same time with the defined class characteristics.  You can also go back and do symmetric or asymmetric meandering to match the lengths, if needed, with the meander command.

There's a good description in the manual and the on-line help.

I'm in the same predicament.  Eagle is dead to me.  Looking to try Kicad.

[rx8pilot]

I have tried the meander tool and it is comedy gold. A truly fiddly thing.

On 5-10Ghz traces - I have to radius the corners. Since doing that during the routing is nearly impossible, I have to manually add a radius to each bend. Meh, whatever, I can get past that. What really makes it useless (unless I am missing something) is trying to push that trace around later. They become just regular traces and the rounded corners go crazy.

In KiKad - is it possible to push and edit a previously routed differential trace and maintain the correct geometry? Is the equivalent of the meander tool have any real control?

[hermit]

Looking to try Kicad.

It is in feature freeze at the moment with a new version due out soon so if you haven't started don't get too far.   Decent forum help available.

[latigid on]

I had no joy with differential traces in EAGLE 7.x. I just have a few short runs of USB, so nothing too strenuous, but I thought it best to try and match them. I never paid for the autorouter, so I'm not sure if the meander tool works.

RUN LENGTH x y , where x and y are the signals to match, then meandering manually with MITER or MOVE works albeit crudely.

[rachaelp]

I never paid for the autorouter, so I'm not sure if the meander tool works.

The MEANDER command is just a regular board command, it's not part of the autorouter so you should be able to use it.

Best Regards,

Rachael

[rx8pilot]

Is Altium the closest step to having routing tools for differential routing? If I have a design where I have to run a bunch of lines, it will consume nights and weekends. 

[Deridex]

Is Altium the closest step to having routing tools for differential routing? If I have a design where I have to run a bunch of lines, it will consume nights and weekends. 

I think the Circuit-Studio can also handle differential pairs, but i'm not 100% sure.

[Bassman59]

In KiKad - is it possible to push and edit a previously routed differential trace and maintain the correct geometry? Is the equivalent of the meander tool have any real control?

In Kicad, yes, you can push previously-routed pairs and they maintain their geometry. Dunno about curved traces, though.

[rx8pilot]

In Kicad, yes, you can push previously-routed pairs and they maintain their geometry. Dunno about curved traces, though.

Well - that is a step up from Eagle!

[macegr]

KiCAD doesn't have curved traces at all, which does really hurt.

[ahbushnell]

Is Altium the closest step to having routing tools for differential routing? If I have a design where I have to run a bunch of lines, it will consume nights and weekends. 

I think the Circuit-Studio can also handle differential pairs, but i'm not 100% sure.

It does handle diff pairs.

[rx8pilot]

Altium is doing a $495 deal for Eagle users. Wonder if now is the time to bail out of Eagle.

Short and misplld from my mobile......

[H.O]

Altium is doing a $495 deal for Eagle users. Wonder if now is the time to bail out of Eagle.

Are you saying EAGLE users can now get Altium Designer for $495 (!?) or is it the Circuit Studio deal you're referring to?
They've been selling that (Circuit Studio) for $495 for quite some time now (EAGLE license or not), at least since Mars -17.

[rx8pilot]

Altium is doing a $495 deal for Eagle users. Wonder if now is the time to bail out of Eagle.

Are you saying EAGLE users can now get Altium Designer for $495 (!?) or is it the Circuit Studio deal you're referring to?
They've been selling that (Circuit Studio) for $495 for quite some time now (EAGLE license or not), at least since Mars -17.

Sorry, I was not clear....just CS.

The page indicates it is only available to Eagle users *FOR A LIMITED TIME* (not sure how they would verify). Either way, CS seems like an upgrade from Eagle overall. My biggest fear is an unknown learning curve. As much as Eagle annoys me, I know it well and have a library that is tied into my MRP and assembly. My guess is that moving over would be a considerable effort.

At the moment - I am a few mouse clicks from design to having the pick and place machine programmed. Not sure what I would have to do with CS to get a similar result.

[H.O]

I'm not doing nearly as advanced stuff as you but I was fairly fluid in EAGLE.
However, when they went subscription (after "promising" not to) I went to Circuit Studio. I jumped on the "limited" offer of $495 back in Mars/April, have barely used it though but it has imported EAGLE schematics, PCBs and libraries when I've tried. I suggest you download the trial and just open one of your EAGLE boards and see how/what it does.

As far as all the custom scipts and ULPs, I'm not sure CS has that capability - at all. I'm sure some will argue you don't need it (or should not need it) but we all know that's a nice thing to have in EAGLE.

[rx8pilot]

I'm not doing nearly as advanced stuff as you but I was fairly fluid in EAGLE.
However, when they went subscription (after "promising" not to) I went to Circuit Studio. I jumped on the "limited" offer of $495 back in Mars/April, have barely used it though but it has imported EAGLE schematics, PCBs and libraries when I've tried. I suggest you download the trial and just open one of your EAGLE boards and see how/what it does.

As far as all the custom scipts and ULPs, I'm not sure CS has that capability - at all. I'm sure some will argue you don't need it (or should not need it) but we all know that's a nice thing to have in EAGLE.

Just downloaded the trial. 10mins later it had imported one of my Eagle projects perfectly - stunned. They clearly saw the value in developing transition tools.

A bit lost in the interface so I will read/watch the getting started stuff. It instantly feels like I just went from a 1990 Honda Civic to a brand new BMW. Hopefully, it won't take long to be able to test the differential routing tools.

[Fire Doger]

CS has output job too, which can export much more than Gerbers and P&P with a few clicks
As an old Eagle user and now AD I had some hard time to jump, it took me 2 weeks to layout something meaningful. CS is more friendly than AD and you look more experienced than me when jumped so I guess in 1 week you will be up n running. Setting templates, output jobs, default rules etc may take some time and hundred of new shortcuts.

Scripts are used in special occasions like importing image, drawing spirals etc

You should definitely try CS but be prepared to spend some time to explore it before trial expires.

I bough a couple of courses from Fedevel Academy. He has some videos (1h long ea) in Youtube about high speed (parts from courses) and a cheap (10$ on sale day) course in Udemy designing from scratch and generating all documents. (links below)
Also DDR, multilayer, rules etc are available but all of them are for AD, I haven't checked CS to confirm if they are 100% same but you can check them out to take a sample of workflow in Altium kind EDA and maybe they will help you out be up n running faster.
Have fun

https://www.youtube.com/channel/UCJQkHVpk3A8bgDmPlJlOJOA
https://www.udemy.com/learn-to-design-your-own-boards/learn/v4/overview
https://www.fedevel.com/academy/

[Macbeth]

You can try CS free for a month. Admittedly that means nothing compared to the time and effort involved in learning it. However I found it much easier than KiCAD - the schizophrenic KiCAD GUI seems to be something nobody wants to address.

As it happens my CS expired a few days ago. There is no need for the cloud connection, it still runs standalone, and what surprised me was I expected the Cloud services like Altium Vault to be closed to me but it's still working.

Having said that my PCB design is pretty much hobby 1 or 2 layer etch at home stuff. CS is wasted on me but I won it in the EEVBlog comp last year. Differential pairs are not something I've had to deal with yet.

Just run CS trial in a VM and sign up for another new trial if you don't have the time in the month to evaluate/learn it. I imagine the $495 price is peanuts if you decide to go for it commercially.

[rx8pilot]

I imagine the $495 price is peanuts if you decide to go for it commercially.

True - the $495 is a marginal component of the decision. The past month has been rapid-fire design which is unusual for me. My guess is if the learning curve is anywhere close to a week to become functional - that is worth it. I watched many of the videos to get a sense of the capability. Without too much surprise - it seems to be ridiculously better than Eagle. It will also provide a simple skills transition to AD if I go that far. 

What I have figured out in an hour (not mastered, just discovered)

Works with my space mouse - AMAZING
3D view!!!!!
Flip PCB to the back side.
push/shove routing
obstacle avoid routing
multi-net routing
easy creation and editing of diff pairs
dead simple import of my Eagle data

This is looking pretty good so far and I was only hoping for a step up in differential routing.

[rachaelp]

Flip PCB to the back side.
push/shove routing
obstacle avoid routing
easy creation and editing of diff pairs

To be fair to EAGLE, as of 8.5.0 and the inclusion of Push & Shove, which was released yesterday, over the last few releases Flip PCB view (8.4.0) and obstacle avoid routing (8.1.0?) are all now available, and EAGLE has done creating of diff pairs for a while. Granted editing isn't ideal, it could definitely use some more polish there. Also in 8.4.0, SPICE simulation was integrated into EAGLE with the inclusion of the ngspice engine. So, regardless of what people think of Autodesk, EAGLE is progressing faster than in has for an awful long time.

With regards to the SpaceMouse, I wish it had proper native support. I have managed to get it to work to a point in EAGLE (on macOS) but it's far from perfect.

If CS works for you and you are happy with it that's great. EAGLE isn't for everybody with the subscription licensing, but then CS isn't for everybody either. To be fair I have never used Altium products, I have used DxDesigner, OrCAD, and some older Mentor Graphics products too. Compared to all those, once I learned (and I mean really, properly, thoroughly learned) EAGLE I became far more productive than in any of those tools.

I suppose I should install CS in a VM and get a trial license so I can have more understanding of what it offers....

Best Regards,

Rachael

[rx8pilot]

I am very impressed with the efforts being put into Eagle - but I believe it is a long road to success considering the starting point.

I did download the trial of the latest Eagle to have a play but have not installed it yet. I won't have an opinion formed about which way to go for a bit, but spending just an hour with CS has me laughing at Eagle, even with all the latest improvements.

[KE5FX]

What are the CS file formats like?  The one thing that EAGLE did right, the thing that makes it hard to switch away from, is their XML format. 

I'll go so far as to say I'll never again adopt a CAD tool that doesn't use a human-editable text-based format. 

[rx8pilot]

What are the CS file formats like?  The one thing that EAGLE did right, the thing that makes it hard to switch away from, is their XML format. 

I'll go so far as to say I'll never again adopt a CAD tool that doesn't use a human-editable text-based format.

Not sure, but I have also never made any real use of Eagle's XML format either. How do you see that as a feature?

[KE5FX]

What are the CS file formats like?  The one thing that EAGLE did right, the thing that makes it hard to switch away from, is their XML format. 

I'll go so far as to say I'll never again adopt a CAD tool that doesn't use a human-editable text-based format.

Not sure, but I have also never made any real use of Eagle's XML format either. How do you see that as a feature?

Just as a few examples off the top of my head:

• Having always done diff-pair routing manually in the past, I decided to try the meander command out for the first time when you raised the question.  My work-in-progress has 128 signal lines, so going back and renaming every one of them with _N and _P suffixes would have been time-consuming.  Instead, I just pulled up the .brd and .sch files in a text editor and did the job instantly with a simple search/replace macro.
• The same technique comes in handy for error-free replication of multi-pin connectors and buses -- just copy the component instance and rename the lines from ADC0_xxx to ADC1_xxx, or whatever.
• My homebrew BOM generator tool works by loading the project's .sch file, enumerating the parts, and cross-referencing them against a master parts database.  Lots of people have written BOM tools in EAGLE's scripting language, but my particular tool is really a small-scale enterprise resource planning app.  It has to interact with other tools and applications, generate Excel spreadsheets, that sort of thing.  Direct access to the .sch data hierarchy from an external C/C++ application is a must.
• The EAGLE authors have made several half-baked attempts at hierarchical design and layout reuse, but as far as I'm aware, they are still nowhere near ready for prime time.  As with my ERP tools, I was able to write a custom tool to do exactly what I needed, again without wasting time with a proprietary scripting language.
• I've lost track of the number of times I've cut and pasted schematic sections from one design to another, only to realize later that I've made my design dependent on random libraries scattered all over the place.  It only takes a few minutes in a text editor to change all of the .sch and .brd files to refer to the same parts in my project-specific .lbr file.  I've never found an officially-supported way to do that other than by manually replacing each individual part.

Many of these shenanigans wouldn't be necessary in a better-engineered application, but I'm well aware that other EDA packages have quirks and annoyances of their own.  EAGLE figuratively gave itself a new lease on life with the XML format, and now that they literally insist on leasing it, I need to move to a new tool with similar capabilities.  An open file format is definitely a requirement, now that I've personally seen how important it is.

[rachaelp]

Not sure, but I have also never made any real use of Eagle's XML format either. How do you see that as a feature?

There are a few advantages of the XML file format:

1) If for any reason you needed to migrate data to another system, with it being in XML format its far easier to parse and extract the relevant data. From this perspective it's more about future proofing your data. If it's in some proprietary binary format, you're a lot more stuck to transfer your data elsewhere.

2) It makes it easier to write utilities to integrate EAGLE into other parts of your system.

3) If for some reason there is a corruption in the file causing a error, it is possible to open, edit and manually fix the issue.

4) If you want to create a new library with a large number of components, say with a known range of values, then you can do this more easily by either using a text editor or writing a utility to generate the .lbr file with all the parts with all the values. E.g. a comprehensive passives library with a number of parts in a range of packages and standard values.

5) Version control systems work with XML files. I use GIT extensively and I can use it with EAGLE files easily.

There are probably other advantages too which I haven't thought of right now.

Best Regards,

Rachael

[rx8pilot]

Those are legitimate uses - thanks for pointing them out. The XML format and ULP API definitely opens the system for unique solutions and applications. Like you said, the fact you need it implies the software is incomplete and requires the end users to figure out on their own how to get the finish line.

When compared to a solution that does not need special development except for the most extreme corner cases - it looks un-appealing to me. I am VERY thankful for EAGLE since it is what allowed me to get started for a low cost. Altium Designer (at the time) was over $10k and I was a total beginner at PCB layout.

Holding my final thoughts until I have a go with the latest version of Eagle. Like it was mentioned earlier, Autodesk is pouring a considerable effort into it.

[rachaelp]

Those are legitimate uses - thanks for pointing them out. The XML format and ULP API definitely opens the system for unique solutions and applications. Like you said, the fact you need it implies the software is incomplete and requires the end users to figure out on their own how to get the finish line.

I look at it like it’s offering me to customise it to work efficiently with my workflow and I can easily make it work in a way that makes me very productive. But this level of commitment to customisation isn’t for everybody. Even so you can definitely use it perfectly well straight out the box once you’ve properly used it.

Other tools aren’t without needing customisation but they make it harder to do it. I used to use DxDesigner and I was incredibly frustrated by the insistence of a 1-to-1 symbol in to package pad relationship. So depending on what package I chose for a FET determined what symbol I used. I wanted standard FET symbols and just be able to map the pins to the appropriate package pads whether it be one or many, and don’t get me started on the stupidly large symbols which were required for power/ground pins on CPUs and FPGAs.... in the end I wrote an entire system external to DxDesigner including a very complicated netlist post-processor to do the mapping based on a load of mapping files which I created as part of my library so that the pins of my sensible symbols were correctly mapped to the correct number of package pads in PADS...

I can’t nelieve how quickly thinking about DxDesigner got me irritated and ranty...., Sorry! 

Best Regards,

Rachael

[rx8pilot]

I can’t nelieve how quickly thinking about DxDesigner got me irritated and ranty...., Sorry! 

Once you have a bad experience with software.....it can boil to near rage. I have a long list of rotten experiences with big $$ professional software that is crap. The vendors go-to solution is always to 'upgrade' to the next level for a pile of cash. Never seems to work.

I have been a Solidworks owner since 1998 - it just works. They are always improving. A couple of bumps here and there, but overall - amazing. I want that same experience for PCB design. Eagle is so close....yet so far.

Subtle things I have noticed (among many) just in an hour.....
Hovering over a net highlights the whole net so you get a visual cue of what your routing needs to do. You can lock 45's and verticals super simple. Exported a STEP file (no random ULP) that went directly into SolidWorks so I could work out the heatsink based on MOSFET locations.

As for diff-pair routing.....still learning obviously. I was able to route easy enough, the setup is easy. The routing is much easier to control overall. Still trying to figure out how to edit/modify a diff-pair afterward. Seems to default to moving a single track although both tracks in the pair are highlighted.

For now, I had to put it away and get back to work. The boards I am working on now are fairly simple, so no major rush. Back to high-speed stuff in a couple of weeks.

[rachaelp]

I can’t nelieve how quickly thinking about DxDesigner got me irritated and ranty...., Sorry! 

Once you have a bad experience with software.....it can boil to near rage. I have a long list of rotten experiences with big $$ professional software that is crap. The vendors go-to solution is always to 'upgrade' to the next level for a pile of cash. Never seems to work.

Yeah that was always the problem I found. They won't talk to you until you've upgraded to the latest version but then even if they do agree it's a bug, you likely won't see a fix for a long time. As for feature requests, rather than the developers taking each idea they see on its own merit and deciding whether to implement it, you just get told to "suggest it on the Mentor Ideas website" and you put it there, amongst the literally thousands of other suggestions where it may pick up a few votes until it drops off the first few pages because there are so many suggestions coming in, then it no longer gets seen because people only read the first page or two so no more upvotes and then your out of luck....

I have been a Solidworks owner since 1998 - it just works. They are always improving. A couple of bumps here and there, but overall - amazing. I want that same experience for PCB design. Eagle is so close....yet so far.

Have you registered on the Autodesk EAGLE forums and posted your suggestions for EAGLE improvements over there? The developers and senior management are quite active on that forum as well as Jorge and Ed who always respond to suggestions made there. I've seen a number of things that have been suggested there make it into one of the Autodesk releases so they are listening and acting upon suggestions now.

Subtle things I have noticed (among many) just in an hour.....
Hovering over a net highlights the whole net so you get a visual cue of what your routing needs to do. You can lock 45's and verticals super simple. Exported a STEP file (no random ULP) that went directly into SolidWorks so I could work out the heatsink based on MOSFET locations.

I think Autodesk are concentrating on getting the EAGLE<->Fusion360 integration to be their primary MCAD integration. Once you get a board into Fusion360 though I'm sure you can export it as STEP at this point if you want to go into SolidWorks. I would be happier if the 3D model of the board was created in EAGLE directly by adding STEP files for components and having a 3D view there which could then be exported to Fusion360 for inclusion into a larger mechanical design or alternatively STEP to go elsewhere. I'm hoping it'll move more in that direction.

As for diff-pair routing.....still learning obviously. I was able to route easy enough, the setup is easy. The routing is much easier to control overall. Still trying to figure out how to edit/modify a diff-pair afterward. Seems to default to moving a single track although both tracks in the pair are highlighted.

Yes, the diff pair routing does need some work to make it a polished feature in EAGLE. It could be made less fiddly to draw the pairs in but I think the largest issues are caused when you need to make a change. It's sometimes easier to rip up and re-route. I'm pretty sure they will fix the issues with this though, it seems like quite a major improvement as diff pair routing is quite an important thing for a lot of people.

For now, I had to put it away and get back to work. The boards I am working on now are fairly simple, so no major rush. Back to high-speed stuff in a couple of weeks.

I could do with a few simple boards, my last few have been quite challenging.... 0.5mm BGA's with dual stacked micro-vias, gigabit Ethernet, lots of impedance matching and length matched nets, etc and of course I had crazy deadlines and people harassing and asking me how it was going every 5 minutes!!

Best Regards,

Rachael

[latigid on]

I tried again with differential routing. I could get the MEANDER tool to work by assigning the trace to length match with Ctrl + click. But there was no real benefit: the meander length was essentially arbitrary. Also, it seemed to generate some sort of UNROUTED trace.

In the end, I found it easier to route the pair as individual traces, add meanders manually and check with RUN LENGTH sig1 sig2.

[rachaelp]

I tried again with differential routing. I could get the MEANDER tool to work by assigning the trace to length match with Ctrl + click. But there was no real benefit: the meander length was essentially arbitrary.

The meander length isn't arbitrary unless you don't specify the meander length.

E.g. If you want to length match a bunch of signals on a data bus to 10cm:

GRID mm;
MEANDER 100

Now drag to meander each of data lines and it gives you a percentage for how close to the ideal length and will limit the length at 100%. I recently finished a 10-layer board with lots of impedance matched and length matched traces and it was actually quite quick and easy to get this done.

Best Regards,

Rachael